V2 Series Work Coordinate System Tutorial (Kinetic Control)

Revision History

Initial Release: November 2021 (MR)

Introduction

In order to properly machine a part it is important to set the work coordinate system (WCS) properly in the CAM software and on the machine. This tutorial explains how to set a WCS origin in Fusion 360 as well as on the machine, using tool touch-offs. This tutorial uses the square part that is produced in the ‘First Part Tutorial (Kinetic Control)', which can be referenced for a more thorough understanding of the full workflow. For this tutorial, a user can use any part that they are milling, and it would be set in the same way just using a different part for reference.

This tutorial uses the Kinetic Control user interface released on 11/1/2021; if you are using the old user interface, please refer to the original version of this tutorial posted under “Legacy Resources”

Section 1: Setting the WCS

To begin CAM programming and create the Work Coordinate System, migrate from the DESIGN workspace to the MANUFACTURE workspace in Fusion. To do this select the “Change Workspace” drop down tab at the top left of the screen, then select MANUFACTURE.

Next, directly to the right of the workspace button reads a button called ‘Setup’. Click this and select ‘New Setup’. The Setup is a tool for Fusion 360 to understand excess material, objects to avoid and the machine's initial position. (To edit an existing setup, right click on it and select edit).

From here, a box pops up on the right hand side that is called “Setup: Setup1”. Within this box is a section titled ‘Work Coordinate System (WCS)'. Select the WCS dropdown next to “Orientation” and choose “Select Z axis/plane & X axis”. The “Machine” field should be left blank so that is says “Select…” and the “Operation Type” should be set at “Milling” as shown below:

Two pieces of geometry will need to be selected to complete the “Orientation” field, one for the Z Axis and one for the X Axis. The Z-axis will always need to point towards the spindle to match the physical machine’s +Z direction. For this tutorial we will start with the oval side facing the spindle. To do this, select the box next to “Z Axis” with a mouse in it, then select geometry (a straight line) on the part that aligns with the axis of the spindle as shown below. If the blue Z-axis shown does not point away from the part and towards the spindle, select the box labeled “Flip Z Axis”:  

Repeat this operation for the X Axis, selecting a feature that runs front-to-back along the part. When finished you should have a WCS that looks like the image below with Y pointing up and X pointing rear. (On the Pocket NC, the Y Axis moves the table up and down, this must be reflected in the setup for the output code to work with the machine). If you need to change the directions of the axes, use the “flip _ Axis” check boxes to flip them.

The orientation of the B axis is flat or (perpendicular) to the spindle of the Pocket NC when homed. This needs to be reflected by the WCS.  On the Pocket NC, the Y Axis moves the table up and down this must be reflected in the setup for the output code to work with the machine. The positive Y direction of the WCS should point straight up from the the B table.

Next, you will select the origin for the toolpaths. The origin will be placed on a corner of the stock so that we can locate it in X, Y, and Z using the machine.

In the Setup menu change the Origin type to “Stock box point.” Then select a corner of the yellow box (which represents the stock material) that is at the top, faces the spindle, and will be positioned near the front of the machine where you can see it.

 

 

If you do not have any fixturing or other parts in your model, you can leave the “Model” section as the default selection “Body”. You can also leave the “Fixture” box unchecked if you do not have a fixture modeled. (If you had fixturing in your model, you could turn on this selection and differentiate between the part and the fixture to help ensure you do not cut the fixture). The first tab of the Setup window should look like the following when complete: 

Next, click on the “Stock” tab of the Setup settings window. This is where the size and position of the stock (the block of material out of which the part will be machined) are defined.

First choose the shape of your stock for the stock mode - the most common options used are “Fixed size box” and “Fixed size cylinder”. (This tells Fusion that the stock is either a cube or rod of known dimensions). The example part below was made from a 2 x 2 x 2 inch block of wax so the “Width” “Depth” and “Height” of the stock were set to 2 inches. Fusion will automatically center the stock boundaries around the geometric center of you parts, but you can add offsets to move the part to a different position within the stock.

For efficiency, it is always best to move your part close to the top of the stock or one of the sides. This will minimize the amount of material you need to remove from that side and will leave more stock remaining after the part is complete to reuse. Positioning the part away from your fixturing will also provide more clearance between the spindle and fixture during cutting.

Next, move to the final tab of the Setup named “Post Process”. Here you can give your program a name and comment as well as pick what WCS offset you want to use. In this example, we are using WCS offset 1 because we want to use the G54 code to define our work offsets on the machine.

When finished in the “Post Process” tab, click OK to save and apply all the changes to the Setup you just created. Save your progress.

Section 2: Creating Toolpaths

After you have finished your setup, create all of the toolpaths for your specific part before continuing. If you would like to see examples of creating toolpaths, please refer to the First Part Tutorial (Kinetic Control).

Section 3: Post Processing

After you have created all of your toolpaths for your part, you are ready to Post Process and create G-code from the the toolpaths. This is the process that Fusion’s software uses to transform the toolpaths into code that the Pocket NC can use.

The toolpaths may be post processed (“posted”) individually or several of them may be selected at once and post processed together. It may be helpful to post process your programs one toolpath at a time until you are confident that they are doing what you want them to do. It is much easier to troubleshoot smaller programs than large ones.

Once you are sure that they are working correctly, it will save time to group as many toolpaths together as possible by posting all of the paths that use the same tool and the same stock setup together.

Post process a single toolpath by clicking on it and then clicking “Actions” > “Post Process”. Alternatively, you may right-click on the toolpath and select “Post Process” from the menu. To post process all of the toolpaths, click the setup (with the default naming “Setup1”) then select “Post Process” using either one of these methods.

Once you click the “Post Process” button, a dialogue box will appear where you can choose which post processor to use, which machine model to use (V2-10 vs V2-50), and add comments to the code. You must select the Kinetic Control post processor from the list and then the machine model. If you do not see the Kinetic Control post processor, please jump to section 5.1 of the First Part Tutorial (Kinetic Control) to learn how to enable this. (Every CNC machine has unique geometry, speeds, number of axes of motion, and other boundary conditions, so every machine has a slightly different post processor. The code will not work correctly on the Pocket NC mill if it is not written with the Pocket NC post processor. Once you select this once, it should stay as your default)

Any program comments that you add here will be added to the beginning of the code. They will not be executed by the machine. This is good place to record the part name, revision number, date, the code’s author etc. for future reference. You will also need to select WCS number 9 (G59.3) from the list next to “Rotated Work Offsets WCS” and enable “Use TCPC mode”. You can also adjust your “Output Folder” to change where the file will be saved. When done, you Post Process window should look exactly like below (unless you changed the Program Number or Comment):

Once you have selected the correct post processor, machine, Rotated Work Offsets WCS, and enabled TCPC, click “Post.”

Your computer’s file browser will open asking you to name the program file (it will also allow you to change where it will be saved). Give the program a descriptive name. The file extension should be left as .ngc. The file should be written to either a local file directory on your computer or a removable storage de such as a USB flash drive.

Click “Save” to post process the toolpath and write the G-code file to the specified location. You can open the file with a text editor program to verify your program number, program comment, and the tool used. (You can also edit your G-code here, just remember to save it afterwards).

Section 4: Locating Rectangular Stock with Work Offsets

Once you have installed your stock and fixturing, you are now ready to locate the stock with respect to the machine. Once the machine knows where the physical origin is located, it can then accurately cut the part from the stock. In this example, we set the origin to the front, top corner facing the spindle. We will want the machine origin to match our CAM:

 

 

There are several ways to locate the origin but in this example we are going to use the simple touch-off/paper method. If you have not done so yet, measure the tool that will be used for this program on the “Setup” tab of the User Interface (UI). With the tool measured, we want to make sure that it is active. Under the “Work Offsets” section at the top of the Setup tab, the tool you are using and just measured should be listed as active and the tool length offset should be listed below it:

If the tool is not active, navigate to the “Manual” tab and type “G54 G43 H18” into the MDI command bar and press enter on the keyboard (use “H18” if you are using tool #18; use “H10” is using tool #10). After this, return to the “Setup” tab and confirm the tool is active.

Now that our correct tool is active, we will begin to “touch-off” the tool on three sides of our origin corner and figure out its position. We will start with the Z-axis.

Setting Z Work Offset

  • Begin by using the jogging controls in the user interface to position the touch-off tool near the right side of the stock, inside the front face and below the top of the stock.

  • Then, using .01” steps, jog the tool towards the stock in the Z negative direction. Be careful not to go too far and collide the tool with the stock. Once the tool is as close to the stock as it can be using .01” steps, insert and hold a thin piece of paper between the tool and the stock. Now switch to .001” steps and continue to move the tool in the Z negative direction until the paper has been pinched.

Note: Using a step size of .0001” to move towards the stock and pinch the paper could be done for a more accurate touch-off. If you know the thickness of your paper, you can also remove the paper after contact and then jog in by this amount for higher accuracy.

Lastly, set the Z work offset by navigating to the “Work Offsets” section of the of the “Setup” tab in the user interface and clicking on the input box in the Z row and G54 column.

  • A pop-up window will appear that allows you to set a value for the current position. Leave this as the default of 0.000in and click the “Set” button.

  • In this example, Z made contact at 0.9900in - your value will differ due to stock size, stock placement, and tool stickout. Note that after setting the Z DRO value to 0.0000, the G54 offset value became our 0.9900in touch-off location and the current Z position is now the value 0.0000in. This means we have set our Z origin to that face, just like we had done in the CAM portion.

Setting X Work Offset

  • Begin by using the jogging controls in the Pocket NC user interface to position the touch-off tool in front of the stock and just below the top of the stock.

  • Then, using .01” steps, jog the tool towards the stock in the X positive direction. Be careful not to go too far and collide the tool with the stock. Once the tool is as close to the stock as it can be using .01” steps, insert and hold a thin piece of paper between the tool and the stock. Now switch to .001” steps and continue to move the tool in the X positive direction until the paper has been pinched.

Note: To learn how to use an edge finder during the X and Y touch off portions, please refer to the Appendix at the bottom of this tutorial.

  • Lastly, set the X work offset by navigating to the “Work Offsets” section of the of the “Setup” tab in the user interface and clicking on the input box in the X row and G54 column. A pop-up window will appear that allows you to set a value for the current position. Since we want to find the true location of this side, using the center axis of the tool, we will need to enter a value to account for the radius of our tool (the centerline of our tool is currently a tool-radius’s distance from the edge of the stock). For the 3mm Datron Tool #18, enter a value of -0.0590in to account for the tool radius (enter -0.0625in if using the 1/8” Tool #10) because that is how far the center of the tool is offset from the face of the stock in the negative direction and click the “Set” button.

Setting Y Work Offset

  • Begin by using the jogging controls in the Pocket NC user interface to position the touch-off tool on top of the stock near the front corner of the stock.

  • Then, using .01” steps, jog the tool towards the stock in the Y negative direction. Be careful not to go too far and collide the tool with the stock. Once the tool is as close to the stock as it can be using .01” steps, insert and hold a thin piece of paper between the tool and the stock. Now switch to .001” steps and continue to move the tool in the Y negative direction until the paper has been pinched.

Note: To learn how to use an edge finder during the X and Y touch off portions, please refer to the Appendix at the bottom of this tutorial.

  • Lastly, set the Y work offset by navigating to the “Work Offsets” section of the of the “Setup” tab in the user interface and clicking on the input box in the Y row and G54 column. A pop-up window will appear that allows you to set a value for the current position. The value used in this example will be +0.0590in for tool #18 (+0.0625 for tool #10) because that is the radius of the tool we are using, which means that is how far the center of the tool is offset from the face of the stock in positive direction.

Note: Including the thickness of the paper in the new DRO value could be done for a more accurate offset.

It is always good to verify that your offsets are in the correct direction and the origin is in the correct location. To do this, retract Z away from the stock, then carefully jog X and Y to their 0.000 positions. After that, slowly jog Z to its 0.000 position. If everything axis is correct, the 0,0,0 position will put the end of the tool centered on the origin corner and just touching it.

Section 5: Simulating with Offsets

Tip: Now that you have a measured Tool Length Offset and Work Offsets, it is a great time to check out the Pocket NC Simulator and simulate your G-code on the actual Pocket NC! You can simulate your program in the newly updated Pocket NC Simulator by uploading the g-code, pressing the stop button and then inputting your TLO and Work Offset values in the summary tab. More details on how to use the Pocket NC Simulator can be found in this video.

Once the simulation looks correct for your part and you have verified there are no errors or crashes, you are ready to cut your part! As a reminder, if you would like to see a more detailed explanation of these steps please refer to the First Part Tutorial (Kinetic Control). The First Part tutorial is great for users that are new to machining or want to understand all of the details.

Happy Machining!

 

Appendix A: Locating Cylindrical Stock with Work Offsets

The ER40 Fixture can be used to fixture cylindrical stock in the center of the B-table. While there are no corners to touch-off for X, Y, and Z, it is actually much quicker to locate cylindrical stock and set up Work Offsets. This is because you only need a Y Work Offset. To begin, use the center of the cylinder’s top face as your Setup Origin in CAM:

 

 

When the machine uses its default origin and does not have an X Work Offset set, X0 will align with the center of rotation for the B-axis. Since the ER40 Fixture and the cylindrical stock are centered with the B-axis, our Setup Origin’s X0 in CAM already matches the machine’s X0. In this case, we do not need to add an X Work Offset or touch-off the stock for the X-axis.

After a tool has been measured to create a Tool Length Offset for Z, the end of the tool will be at point Z0 when it is centered with the B-axis as well. Since our Setup Origin in CAM also has Z0 at the center of the stock and thus, the center of the B-axis, we do not need to touch-off in Z or create a Z Work Offset.

With X and Z already accounted for by the machine’s default settings and without work offsets, all you will need to do is perform a Y touch-off on the top of the cylindrical stock to create a Y Work Offset. (Don’t forget to adjust for the radius of the touch-off tool).

Appendix B: Using an Edge Finder

An Edge Finder (such as the one used in the Pocket NC V2-10 Edge Finding Tool Holder) can be used to more accurately locate stock than the paper method. This is because the precision tip has a solid edge and provides visual feedback when it makes contact. (These tools work best when touching off in the X or Y axis; it is not recommended to use an edge finder to touch off in the Z axis).

The process for using an edge finder is very similar to the process above that uses a cutting tool. First, start by bumping the end of the edge finder so that it is not concentric with the shank. Then, turn the spindle on to 1000rpm by entering G0 G90 M3 S1000 in the MDI command line on the “MANUAL” tab of the user interface.

Do not exceed the maximum speed for which the edge finder is rated. For the Pocket NC the maximum operating speed is 2000 rpm. Exceeding this speed is dangerous for the operator and is likely to cause damage to the tool.

Move the tool towards the face you want to locate, stepping in smaller increments as you get close, just like previously described in this tutorial. As the tip starts to touch the face it will start to spin more concentrically with the shank of the edge finder. Keep moving the edge finder toward the part until the tip spins concentrically with the shaft of the edge finder. Continue to move the edge finder closer to the part until you see the tip suddenly “jump” to a new position that is no longer concentric with the shank of the edge finder, this is the contact position. At this point, you can click the “RESET” button at the bottom of the screen to stop the spindle (or enter G0 G90 M5 in the MDI command line to stop the spindle).

Look at the value in the Digital Readout (DRO) to view the current location and set the work offset just like described above for the X and Y work offset. In this case, we will need to account for the radius of the edge finder (where previously we had accounted for the radius of the cutting tool). The radius of the PNC edge finder is 0.100”. All other steps of using an edge finder are exactly the same as described above with a cutting tool.

Happy Machining!